- **OpenFOAM**
(*https://www.cfd-online.com/Forums/openfoam/*)

- - **Boundary condition for bifurcated flow**
(*https://www.cfd-online.com/Forums/openfoam/80341-boundary-condition-bifurcated-flow.html*)

Boundary condition for bifurcated flowDear all
Does any one have experience on simulation of bifurcated flow - flow with one inlet and two outlets. I am trying to run a simulation of bifurcated blood flow and just wonder what will be the appropriate boundary condition to use. I have the information for inlet pressure & velocity, tow outlet pressures. What I implemented so far is to specified the pressure boundary condition only and let the OpenFOAM to evaluate the flux normal to the patch with pressureInletVelocity. Inlet: U with pressureInletVelocity (value uniform (0 0 0)), p with fixed value of P1 Pa/kg/m^3 outlet1: U with inletOutlet (uniform (0 0 0 )) p with fixed value of P2 Pa/kg/m^3 outlet2: U with inletOutlet (uniform (0 0 0 )) p with fixed value of P3 Pa/kg/m^3 wall: U with fixed value (uniform (0 0 0)) p with zeroGradient However, the simulation seems to be highly unstable. Is there anyone know a better way to setup the appropriate boundary condition for this type of flow? Thank you very much. |

Change outlet biundary conditionsHi,
I am runing a case with two inlets and two outlets, akin to a cross-slot. At the inlet, I impose the average velocity, and at the outlet I impose zero gradient, ensuring that the flow has enough length to fully developed. For pressure at the outlets I used uniform fixed value equals to zero. Works great... Titio |

Hi JieJie,
I think a small example illustrates the source of your problem: Imagine an incompressible fluid in a pipe(constant diameter). If you set U_inlet = 100 m/s and U_outlet = 1 m/s, the calculation will crash whatever you do! In your case the pressure on all patches is fixed. But are these values physically correct? If your bifurcation is asymmetric the pressure values at the outlets surely differ from each other. You may did this pressure assumption with regard to the natural original, but: The walls of a blood artery are elastic, so their shape depends to the lokal pressure. Is your model capable to represent this characteristic? Otherwise you can't assume an equal outlet pressure. (But it would be a good verification, if your numerical results fit to that fact.) And I hope you not need to be overprecise or the blood neoplasm overthrow your mass conservation.;) To increase the stabillity (I think it's staedy state?): 1. set a higher number of outer correction cycles for SImPLE 2. use setFieldsDict to guess a near by solution for the fields inside your model. It's easier for the solver to find convergence. 3. You may try a test and change pd_inlet and U_outlet to zeroGradient and see how stable it runs. From numerical point of view defined velocity at inlet and pressure at outlet is the most stable combination. But I would'nt trust the results as long as the pressure on both outlets is fixed. sorry for the big text bests, Robert |

velocities will never workDear All,
Because of the overall mass balance, if inlet and outlet velocities are different, it means the channel dimensions are different. If they are the same, the simulation naturally blews... That is why pressure boundary conditions at the exit are natural. If you want to imposed velocities, you have to used derivatives, otherwise it will be impossible... Titio |

Quote:
what is your pressure condition at the out let? I tired some similar as well. I set velocity at inlet with averaged velocity and at outlet I set zero velocity gradient. For pressure, I set zero pressure graident at inlet and fixed pressure value of uniform 0 at the outlet. However, I found the flow hardly moves in the blood vessel. Thanks jie |

Quote:
Thanks for the reply. The pressure on the two outlets are different, but the difference is very small. Also the cross-sectional area for inlet and two outlets are different, A_inlet > A_outlet1 > A_outlet2. I might need to find more clinical data set for the case I am running. jie |

Hi JieJie,
to know the (measured) pressure values for the outlets is great. But then you shall set the inlet pressure to zeroGradient (otherwise your measurement error would increase instabillity). The case is completely defined with outlet pressure and inlet velocity. If you use an incompressible solver: They are very sensitive to the pressure field. You better set wallBuoyantPressure to the walls not zeroGradient and reduce the tolerance for pressure solution. bests, Robert |

Quote:
I tried constant velocity inlet and zero velocity gradient outlets with zero pressure gradient inlet and constant pressure outlets. However, I found that the flow hardly moves in the bifurcated vessel no matter how big the inlet velocity I use. Cheers, jiejie |

Boundary conditionsHi,
I believe the right conditions for your case are: - Velocity: constant velocity inlet and zero gradient at the outlet. This means that the flow is fully developed at the outlet. - pressure: zero gradient at the outlet and fixed value, say zero at the outlet. OpenFoam calculates the pressure relative to the exit pressure. Questions such as variable tube diameter can be taken into account using this boundary conditions. For pipe flow the previous conditions work like a charm to me. Regards, António Martins |

Quote:
DO you use both zero gradient and fixed value of zero at the outlet??? or you suppose to say zero pressure gradient at inlet and fixed value of zero pressure at the outlet? Thanks jiejie |

CorrectionHi,
I meant zero pressure gradient at inlet and fixed value of zero pressure at the outlet. Worked hard today. Going to sleep. Is midnight in my time zone..... Titio |

Quote:
The flow noting moving problem is solved. It was due to the orientation used in the previous mesh model. Thanks for help everyone =) |

Gas Turbine combustor inlet conditionsHi all,
Im trying to simulate a gas turbine combustor for which I know inlet conditions (massflow, pressure, temperature) and I want to evaluate efficiency of the combustor based on the outlet conditions.I have experienced that OF blows up whenever I specify at the inlet (fixedValue BC) either: a) temperature pressure and velocity (T p U - fixedValue) b) pressure and massflow (p phi - fixedValue) c) pressure and velocity (p U - fixedValue) The other quantities are set to zeroGradient (note for velocity also used pressureInletValocity) Any suggestions? Thx |

All times are GMT -4. The time now is 05:26. |